CNCGUY, Want to rid yourself of [spaces] in certain places? Here is how -> code: !spaces # Save current 'spaces' setting to 'prv_spaces' spaces = 0 # Turn off spaces *progno, "(EMCO", " ", progname," ",*smonth,"-",*day,"-",*year,")", e spaces = prv_spaces # Restore previous setting

The following are segments from the MPFADAL2.PST -> code: # These formats used only for 'Date' & 'Time' fs2 25 2.2 2.2lt #Decimal, force two leading & two trailing (time2) fs2 26 2 0 2 0t #Integer, force trailing (hour) fs2 27 0 2 0 2lt #Integer, force leading & trailing (min) code: # -------------------- Date & Time Formatting ------------------------------ fmt 25 time2 # Capture 24-hour time value into 'time2' variable fmt 26 hour # Hour fmt 27 min # Minutes # Uncomment the 'fmt' for 'day' and/or 'month' if you only want 1-digit format #fmt 26 day # Day (2 digit format) #fmt 26 month # Month (2 digit format) code: ptime #Turn 24-hour time format into AM/PM format !spaces spaces = zero if time >= 13, time2 = (time - 12) else, time2 = time hour = int(time2) min = frac(time2) *hour, ":", *min, if time > 12, " PM" else, " AM" spaces = prv_spaces

Check out MP_LAUNCH.PST in the forum FTP in the "Text_&_post_files_&_misc folder" Does exactly what PIP was asking about. [ 11-05-2003, 09:30 AM: Message edited by: Roger Martin from CNC Software ]

You could using some brute force programming in the PST. First you would need to select a "special" character to use as an end-of-line delimeter in the Operations Comment box (like '$'). Your comments in the Comment entry box would look something like this -> COMMENT FOR 1st OPERATION $ Line2 $ Line3 $ Line4 $ Line 5 $ Then using the fore mentioned brute force method in the PST, use the STRSTR and BRKSPS string functons in MP to 'break down' the original string to individual (comment) lines. If you are really serious about this (and don't mind you Operation Comment in the toolpath parameters looking 'strange $', let me know and I can supply the PST code example .

Sure it is possible. How - depends on which "Multi Post" you are referring to. The MULTI_POST.PST & MULTI_PST.VBS combo. -or- the MULTIPOST.VBS script that Mick posted on 9/16/2003

You can also do this... *e # Blank line This will get you an EOB [CR/LF] forced out, without adding a [space] to the program.

quote: I see this once in a while psof p__2:925 whats the p__ with nums after it mean ? Postlines between brackets are considered an "implied" postblock by MP.DLL From "Post Debugging Techniques" in the Post Reference Guide documentation -> Bracketed postblocks are identified in debugging by the post line number of the occurrence of the open bracket(starting at zero). In the following example, notice the postline label appended to the output line is p__1:250. N10 G01 X1.0 Y2.0 Z3.0 p__1:250 In this example, p__1 indicates the second occurrence of the open bracket ( [ ) and that the bracket was located on post line number 250.

quote: Roger, should the "spaces" references in the ptoolcomment and psof postblocks also be removed? Not nessesary to do that. The problem ocurred becuase the 'spaces' references in the PTIME postblock were nested inside the 'spaces' manipulations in PSOF. (PTIME gets called from PSOF)

Metal, Just remove the (3) references to 'spaces' in the PTIME postblock. code: ptime #Turn 24-hour time format into AM/PM format # !spaces # spaces = zero if time >= 13, time2 = (time - 12) else, time2 = time hour = int(time2) min = frac(time2) *hour, ":", *min, if time > 12, " PM" else, " AM" # spaces = prv_spaces

Yes, I've gone into great detail with this explanation. Maybe too much for experienced MC users. The Post Dept gets the "My post is not working, I get the Single axis rotation error" a LOT. So I'm not picking on you Nominal This explanation assumes that you are indexing around a part on your VMC. If you do not have a sample drawing, do this to make it easier to see. Draw an 6"x4" rectangle in the Side Cplane centered at the Origin. Set the Gview to Isometric (this just makes it easier to see what you are doing) Xform-Translate (using Join method) that rectangle "-10" in the Z axis. 1> Set the Tplane to TOP. Press ALT-F9 to display the axes. Looks like you would expect... +X axis going to the "right" +Y axis going "out thru the back of the part" +Z axis coming "up" out thru the top of the part 2> Now set the Tplane to '3' Press ALT-F9 to display the axes. Looks like you would expect... if imagine yourself looking down the Z at that face +X axis going to the "right" +Y axis going "out thru the back of the part" +Z axis coming "up" out of the part But wait! When you index to that face (Tplane #3) into the real machining position on your VMC, which way the +X axis pointing? On the machine the +X to the right - correct? Refer to Step #2 above. Look at the axes displayed in MC Notice that in addition of your +Z being rotated (which you wanted), that the +X is pointing in the opposite direction! That gets you the -> quote: Only single-axis rotation is allowed! Angles may be incorrect. Because you have rotated TWO axes going TOP or FRONT into that view. Note that if you just post operations that are in that view, the post will not complain. Everything was in that one view. The post will complain only when going from processing toolpaths in one view to an new view and more than one axis has changed directions. Do you need to use WCS to 'fix' this? NO. People forget that when you click 'WCS' on the menu, you are going into the VIEW Manager. Use the Named View feature! Go into the View Manager. (click on 'WCS') Right click on the 'System View 2 - Front' and select 'Create' and then 'Select menu' Select Rotate, Y+ up, and enter '180' for the rotation angle and click Save. Your are now back on the View Manager dialog. Enter a user friendly name for this view. Now whenever you need to set Cplane or Tplane or Gview to the "back side", just click Tplane, Named and select that Named View.

quote: Only single-axis rotation is allowed! Angles may be incorrect. If you ever see this. It is in your toolpath! You have flipped more than one axis from one operation to the next (check your X axis directions, that is usually the problem). You don't need to be using WCS to make this mistake.

I've uploaded MULTI_PST_VBS.ZIP to the FTP site in the "Text_&_post_files_&_misc" folder. Be sure to read the README in the ZIP! BTW, The RunVBS() to execute a script from within a PST has lots of possibilities. "post" post processing the NC file just created, etc. Or like it is used in MULTI_POST, to gather information to pass to the PST. BTW, If you have MP v9.15 you already have the RunVBS() functionality.

quote: If anyone wants - I can upload the new MULTI_POST.PST & MULTI_POST.VBS that do this to the forum FTP. I will upload this as soon as I get a chance to make it a bit more bullet-proof. I discovered that if you click the CANCEL button on the BrowseForFolder dialog the script logic just continued on - using the "C:Documents and SettingsMy Documents" folder ?!?! This would occur even if the default folder was set to "C:WORK". Not a big task to correct, just didn't have a change to work on it last night. On the bright side I found an option that allows the addition of an Edit Box on that dialog, so you could type in the path if you wanted to.

Mick is way too fast... Millman, it is possible to do it all with some simple changes to your MULTI_POST.PST (you were very close), but your input is limited to ALT-V (pasting) the desired folder path or typing the entire path for the answers to the 'fq' post prompt questions. Not the most friendly. But... If you still would like to use the MULTI_POST.PST method. You can fire off a VBS from within the PST. This will do the 'BrowseForFolder' dialogs. Then the VBS will write these folder paths out to a text file. The PST then can open this file and read in the folder paths. This sounds a lot uglier than it really is! If anyone wants - I can upload the new MULTI_POST.PST & MULTI_POST.VBS that do this to the forum FTP. BTW, 'BrowseForFolder' is a function within the VBS script. (I stole this code from one of Mick's scripts for the MULTI_POST.VBS ) In his 'BrowseForFolder' function his is using the 'BrowseForFolder' method that is in the Microsoft Windows Scripting Host (WScript.exe) - that is why you don't find it in the VBS help.

Are you saying your method does not work? Or you would like a more sophisticated method of inputting the data path (using a dialog box) code: sFOLDER1 "sNETWORK" #This is where the NC file will go sFOLDER2 "sSETUP" #This is where the Setup Sheet will go Note that the above definitions of sFOLDER1 and sFOLDER2 are not want you want. sFOLDER1 "sNETWORK" will load the literal string "sNETWORK" into the string variable sFOLDER1, not the contents of the sNETWORK string variable from the answer supplied by the user input of Question #1

If you feel that is path in incorrect, it should be sent to [email protected] Be sure to include a good sampe MC9 with you explantion. ---- "Was the posted output differnt that the backplot". Many times we get "my pots is bad", when in fact the post is doing exactly what it was told. You may think that a move should be at Feedrate, but if the backplot shows is as a Rapid and that is waht the PST produces - it's not the PST. This does not mean that there may not be problem, but now you know to look elsewhere.

May^Day, Is this really a "post" issue? Is the posted output different (G0/G1) than what the backplot of that toolpath shows?

Load up the MPFAEDAL2.PST that is on the CD Search for "tap_speed" to see the areas that setup the Rigid Tap mode prior to the cycle.

Doing this, you are choking the input into the PST. I never recommend messing with the NCI precision setting. Definitely never set it lower than '5'. If you do... Depending on the math being performed in the PST (trig. calculations, etc), you could see arc output problems, etc. You want to talk about something difficult for tech support to run down! Same PST posting the operations in the same MC9 with the same version of MC, good output on everyone's system EXCEPT the customers. It was finally determined that they had set the NCI precision to '4'. Charles Davis probably remembers that one!

quote: The easiest way is to change the output of the NCI file to 3 places after the decimal. You do this by going to screen/configure/NC setting Do NOT do this !!!

[ 09-22-2003, 05:13 PM: Message edited by: Roger Martin from CNC Software ]

Pip, What is the setting of the user-defined 'sofcom' variable when you get the dupiclated comment output? The rule has always been that you do NO boolean logic testing IN the PCOMMENT postblock. If you look the standard MPFAN.PST would will see this -->> pcomment #Comment from manual entry (must call pcomment2 if booleans) pcomment2 and all the logic tests are done in the PCOMMENT2 posblock. I would suggest relocating the logic test currently in PCOMMENT to PCOMMENT2 Before you do that, try this -->> Turn OFF 'fastmode' and set 'bug2' to 40 Add the "PRINT I AM HERE" # lines into each postblock, like show below -->> This will hopefully allow you do determine which postblock outputs what, then you have a much better chance of finding the problem. code: pcomment3 # only for the C-Hooks psdata "*-> pcomment3 <-*", e #<diag> # scomm = ucase(scomm) # scomm, e pcomment2 # Manual Entry - COMMENTS (on a block by itself) 1005,1006 "*-> pcomment2 <-*", e #<diag> if sofcom = 1, subout = 3 scomm0 = ucase(scomm0) if gcode = 1005, n, "MSG ", scomm0, e scomm0=sblank pcomment_0 # Manual Entry - COMMENTS (on a block by itself) 1005,1006 "*-> pcomment_0 <-*", e #<diag> #if gcode <> 1006, pcomment2 #if gcode = 1006, scomm = sblank pcomment # Manual Entry - booleans with comments must call postblock "*-> pcomment <-*", e #<diag> if gcode <> 1006, pcomment2 pcomment30 # only for the C-Hooks psdata "*-> pcomment30 <-*", e #<diag> if sofcom = 1, subout = 3 scomm0 = ucase(scomm0) n, scomm0, e pscomm0 # Manual Entry - booleans with comments must call postblock "*-> pscomm0 <-*", e #<diag> if gcode = 1006, pcomment30

What I listed are Lathe "MISC OPS" toolpaths (Toolpaths->Next Menu->Misc Ops.) The parameters for each of these Misc.Ops. toolpaths all contain a setting (value) that gets passed to the PST in 'stck_chuk_st_x' Lathe Stock Transfer -> writes 'NCI 900' data which calls the postblock 'pstck_trans' Lathe Stock Flip -> wrties 'NCI 901' data which calls the postblock 'pstck_flip' Lathe Stock Advance -> writes 'NCI 902' data which calls the postblock 'pstck_bar_fd' Lathe Chuck -> writes 'NCI 903' data which calls postblock 'pchuck' For example on the Stock Advance dialog the value set for Stock Position-Original Position (look at the middle-left in the dialobg box) is the value passed to the PST in 'stck_chuk_st_x'

stck_chuk_st_x Variable Type: NCI variable Category: Lathe Misc Ops functions information Description: Initial X axis chuck position Notes: Used with Lathe Stock Transfer function (NCI 900), Lathe Stock Flip function (NCI 901), Lathe Stock Advance (Bar-Feed/Pull) function (NCI 902) and Lathe Chuck function (NCI 903). See related: stck_chuk_st_z

If you are talking about using the .SET type Setup Sheet templates - sure can... From my eariler post -> quote: I did that automatically created a Setup Sheet (using the .SET type setup sheet templates) immediately after the PST has created the NC file. You just posted your operations as usual and you got the .NC and a .DOC with no additional steps.